Hi, I'll give you a screenshot of a document I use for PCB design that gives you temperature rise vs current. To prevent thermal shutdown you need to take in to account your ambient temperature, then add the °C rise of your trace from this chart. If that number exceeds your thermal shutdown temperature you need to increase trace size. One other thing you could do is order the same PCB as with 2oz copper, which effectively doubles the amount of copper. 

BTW, this is how you use this chart. Pick a temperature °C rise you want, match with current. Draw vertical line down to the oz copper the PCB will be (1 is standard). So if you wanted minimal temperature increase at 2.5A (10°C rise) on standard 1 oz copper, you would need a ~40 mil wide trace.

I have not yet found a good reference for calculating via dimensions and placement density (number vs. spacing) to calculate a given thermal resistance.so they still a bit of a guess.

Vias filled with solder obviously conduct heat better than unfilled vias. :)

@cjohnson Thank you for this graph, I never knew such resources existed for PCB design. Looking over my current design makes me think that the trace widths are possibly not the cause of concern of my thermal shutdown issue since my power traces are around 80mils since I used a wide copper pour. Could my thermal vias not be implemented properly in the design here [PCB link](https://easyeda.com/iqasi096/bq24650evm-board_copy) ?

@iqasi096 Personally I would fix the thermal pad plane under U3. Does C22 and R20 need to be directly underneath it? Could they be moved to the top or moved somewhere else so you can have a large thermal plane on the bottom side with more thermal vias on that thermal pad? Maybe change the thermal pad's net to PGND instead, that way it can use the entire bottom plane as a thermal plane?

@iqasi096 Maybe get rid of R20 if you are placing it anyway, that would connect the EP (thermal pad) directly to the PGND plane possibly eliminate the thermal shutdown.

@andyfierman Its a shame since having the via reference would be a great addition :(

@cjohnson so the reason R20 was placed there was due to the design parameters suggested by texas instruments to eliminate noise. It was noted that it has to be directly under the BQ24650 IC. I can however move C22 but not too far from the IC to keep the signal from attenuating

@cjohnson found here [PCB layout guideline](https://www.ti.com/lit/ug/sluu444a/sluu444a.pdf?ts=1598898275148&ref_url=https%253A%252F%252Fwww.ti.com%252Ftool%252FBQ24650EVM-639) on page 9 section 3. The first two points seem very counter intuitive... Is there a misunderstanding/misinterpretation happening???

 This group of 9 vias is the underside of the thermal pad directly attached to the plane. I would use this design

@iqasi096 Excuse my mistake comment. That picture is of one of the inner layers. I think the issue with your board layout is you didn't create planes on the inner layers at all.

@cjohnson Hmmm.... I am slightly confused, I am using a two layer board, are there additional layers which are required to be fed into my current design?? I understand their board is a 4 layer board with heavier copper, but is it not possible to design a two layer board with the appropriate thermal via and trace width precautions to handle currents of up to 2.5 A across the PCB?? I apologize if I am asking some basic questions, its just I have not designed boards which supply currents greater than 1 A and all this is new to me. I am very much obliged for your help

@iqasi096 Your layer manager shows you selected 4 layers so I assumed you just forgot the inner planes. It can probably work just fine with 2 layers but you will need to move that R20 out of the way (or remove it at a sacrifice of noise) and plane it directly.

@cjohnson Oh I understand, I must have forgotten to switch it back to 2 layers after the 3 version of this board was designed and ordered. Thanks I will look into doing that and hopefully that would fix my thermal shutdown problem. Thank you very much! :D

@iqasi096, For info, there are a number of online calculators available, based on the graphs that @cjohnson kindly uploaded. For example: [https://www.7pcb.com/trace-width-calculator.php](https://www.7pcb.com/trace-width-calculator.php) [https://www.4pcb.com/trace-width-calculator.html](https://www.4pcb.com/trace-width-calculator.html) [https://www.desmith.net/NMdS/Electronics/TraceWidth.html](https://www.desmith.net/NMdS/Electronics/TraceWidth.html) [https://www.smps.us/pcb-calculator.html](https://www.smps.us/pcb-calculator.html)

First thing to do is change the default via size to 30/15 or even better 48/24.  24/12 is for low power digital circuits and doesn't conduct either current or heat well to the bottom layer.  Also extend the areas where there is no solder resist significantly.   The actual trace sizes look good though.